Learning Forum

[HarsihilZLHZ]

Static analysis with same Component and loading conditions performed considering bonded contacts . 

Got different values for total deformation and Von Mises Stress using Formulation method such as Augmented, Pure Penalty, Normal Lagrange,and MPC.

Why values are different for deformation and Stresses using different formulation method?

How to interpret the results and which formulation method to go with?

@peteroznewman @SandeepMedikonda

[Rev0]

Hallo this is caused by the different contact technologies.
Pure Penalty: The normal displacement of both bodies is coupled by springs. With higher (contact-) stiffness the relative displacement (gap or penetration) is smaller. Due tue these spings a normal loading is causing an relative displacement between both bodies and therefore the total displacement might be higher than expected. With increasing contact stiffness this error can be reduced, but the convergence behavior will be worse.
Normal Lagrange: This contact works with additional equations, so your total DOFs are increasing. The contact will behave as you expect in reality because there is almost no penetration. The convergence behavior might be worse. Years ago it was hard to solve more complex nonlinear analysis with normal Lagrange, today the convergence behavior is way better.
Augmented Lagrange: It is kind of a combination of both previous algorithms. It has a contact stiffness and can reduce the penetration by additional contact iterations. This should lead to a good convergence behavior in combination with small penetrations. This is the reason why it is the current default contact algorithm within Ansys Mechanical.
I'm talking about contact penetration because the above mentioned algorithms can be used for linear (bonded, no separation) and nonlinear contacts (frictionless, frictional, rough).
MPC (Multi Point Constraint): Can only be used for linear contact behavior. The DOFs of the two bodies are coupled, so your total DOFs are reduced. This is the fastest contact algorithm for the solver. Most disadvantage is the possibility of over-constraints.
This should explain the different displacements. Overall your global stress distribution should be independent of the contact algorithm. Differences at the local stresses close to the contact regions can occur. For a better understanding of your problem some pictures would be helpful. Any suggestions without these are hard to tell. Maybe you can avoid this problem by using shared topology, so the mesh of both bodies is merged.
Ansys Help: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v221/en/wb_sim/ds_contact_theory.html?q=augmented%20lagrange
Regards JB

[bhagwantP]

Hello Rev0,

Thanks for your eloborative answer.